Drill slots are supported from most tools, when used in typical ways. See our Slots page for detailed information.

4 Layer Stackup

The current 4 layer board stackup is as follows:

Thickness

Layer

Tolerance

1 mil (0.0254mm)

solder resist

+/-0.2mil (0.0051mm)

1.4 mil (0.0356mm)

1 oz copper

6.7 mil (0.1702mm)

FR408 prepreg

+/-.67mil (0.017mm)

0.7 mil (0.0178mm)

0.5 oz copper

47 mil (1.1938mm)

FR408 core

+/-4.7mil (0.1194mm)

0.7 mil (0.0178mm)

0.5 oz copper

6.7 mil (0.1702mm)

FR408 prepreg

+/-.67mil (0.017mm)

1.4 mil (0.0356mm)

1 oz copper

1 mil (0.0254mm)

solder resist

+/-0.2mil (0.0051mm)

The substrate for both the core and prepreg is FR408, with a dielectric constant of 3.66 at 1GHz, and is compatible with a lead free process. The boards themselves are also lead free and RoHS compliant.

Layer Naming

When sent to fabrication, the layers are manufactured in the following order according to their file extension. We advise following this naming scheme if your design is sensitive to distance of the inner planes in order to avoid any confusion.

Layer

Suggested File Extension

Layer 1

.GTL

Top or Front layer

Layer 2

.G2L

Internal plane

Layer 3

.G3L

Internal plane

Layer 4

.GBL

Bottom or Back layer

Internal Plane Polarity

When submitting gerbers, we need the “positive” internal planes, meaning that lines represent copper, not the absence of copper.

Some CAD tools will generate the internal planes as power planes with “negative” polarity so the lines indicate where copper should be removed. To work around this, declare the internal planes as signal layers and use a copper pour to define the power plane.